End Mill Advice for CNC

[herromynameis]

Hey friends, I've been looking for a good reference on the essential end mills for CNCing fixed blades. I see countless end mills on makers' tool changers, but have a feeling there is a smaller essential list, similar to grinding belts. Everyone has their version of, "Get yourself a 36 ceramic grit, 120, 220, etc." I'm curious how you would boil this down to maybe 4 or 5 to purchase immediately - For example if I was to guess - A beefy profiling cutter, a refined profiling cutter, a rough beveling end mill, and a fine bevel finishing end mill. Thanks in advance fellas.

 

[HSC ///]

what's your experience milling and programming a CNC?
I'm asking because I think you need more of a "plan"
What's your setup? how rigid?
milling hardened or annealed blades?
I think the cutters answer is easier once you understand your plan to remove the material.

I haven't programmed a CNC mill in many years but I used to, and this is how I would approach milling blades.

 

[shinyedges]

I'm a cnc machinist/programmer, what mill do you have? 40 taper?

Are you going to ball mill the primary bevel?

The more info you provide the better advice that can be given. Tons of great options for doing all those tasks. A smaller hobbiest machine will need to run different tooling than a larger machine.

 

[herromynameis]

what's your experience milling and programming a CNC?
I'm asking because I think you need more of a "plan"
What's your setup? how rigid?
milling hardened or annealed blades?
I think the cutters answer is easier once you understand your plan to remove the material.

I haven't programmed a CNC mill in many years but I used to, and this is how I would approach milling blades.

Hey Harbeer! I was reading your comments on other posts about rigidity and largest dia tool/shortest length etc. earlier and thought your inputs were extremely thoughtful. Thank you for your time. I'll give you a full rundown here and appreciate any and all advice.

-I have veteran experience in Autodesk programs like Revit and Autocad but have not used Fusion 360 as of yet. I've downloaded it and am beginning to learn it through aggressive youtube video intake.
-My plan is to mill annealed 10" max length fixed blades assuming this is more forgiving and possibly quieter than machining hardened steel. After extensive research, the clear reliable choice is a Tormach 440 to start. I would be bringing these blades from profiling to beveling, all the way to kydex sheath work.

 

[shinyedges]

Hey Harbeer! I was reading your comments on other posts about rigidity and largest dia tool/shortest length etc. earlier and thought your inputs were extremely thoughtful. Thank you for your time. I'll give you a full rundown here and appreciate any and all advice.

-I have veteran experience in Autodesk programs like Revit and Autocad but have not used Fusion 360 as of yet. I've downloaded it and am beginning to learn it through aggressive youtube video intake.
-My plan is to mill annealed 10" max length fixed blades assuming this is more forgiving and possibly quieter than machining hardened steel. After extensive research, the clear reliable choice is a Tormach 440 to start. I would be bringing these blades from profiling to beveling, all the way to kydex sheath work.

I recently went down this path and a wise man on bladeforums guided me away from the haas. Instead I picked up a mori seiki. WAY more accurate, better surface finishes through rigidity that dwarfs the tormachs.

Look at the spindle of the tormach compared to the spindle of a haas and then compare the spindle of the haas to a mori.

The tormach 440 is on the far end of hobbiest vs real machine. I know it sucks to hear but it is what it is. I'd grab a haas before the tormach for sure. You'll be limited on the tooling that weak motor can run as well as the rigidity it lacks.

 

[herromynameis]

I'm a cnc machinist/programmer, what mill do you have? 40 taper?

Are you going to ball mill the primary bevel?

The more info you provide the better advice that can be given. Tons of great options for doing all those tasks. A smaller hobbiest machine will need to run different tooling than a larger machine.

Hey Shiny, thanks for the comment, I really appreciate you. I'll be running a Tormach 440, so not a 40 taper. As for your other questions, this is where I start to bow before your Obi Wan. In my research so far, I haven't been able to piece together strong opinions on the best methods yet. My initial assessment is that ball milling the bevel is the way to go unless you tell me otherwise. If you tell me I'm a fool for not using a 1/8" snot-coated ball nose single end mill from a forge in Uzbekistan then I'll order one. I'm planning on getting a TiAlN lakeshore carbide 4 flute cutter (width unsure) for profiling, and that's as far as I've gotten in my list... Because I'm not manufacturing large batches and need the machine fairly quiet, I'm thinking I would run the machine slow and use TiAIN coated and clear chips with air instead of coolant. Hopefully that sounds sensible.

 

[shinyedges]

Hey Shiny, thanks for the comment, I really appreciate you. I'll be running a Tormach 440, so not a 40 taper. As for your other questions, this is where I start to bow before your Obi Wan. In my research so far, I haven't been able to piece together strong opinions on the best methods yet. My initial assessment is that ball milling the bevel is the way to go unless you tell me otherwise. If you tell me I'm a fool for not using a 1/8" snot-coated ball nose single end mill from a forge in Uzbekistan then I'll order one. I'm planning on getting a TiAlN lakeshore carbide 4 flute cutter (width unsure) for profiling, and that's as far as I've gotten in my list... Because I'm not manufacturing large batches and need the machine fairly quiet, I'm thinking I would run the machine slow and use TiAIN coated and clear chips with air instead of coolant. Hopefully that sounds sensible.

We all start somewhere! It's a journey/ learning experience, I'm a machinist/programmer by trade but not experienced in machining knives specifically, so a mentor/friend of mine who is machining knives has been invaluable. The tormach has .75 hp, and the rigidity of a noodle. The r8 taper is tiny and not for serious work. That's your biggest limiting factor in tooling. So if you haven't got it yet, I'd recomend against it. If you have, then you'll need to work around the very serious limitations you'll have with the tormach.

 

[herromynameis]

I recently went down this path and a wise man on bladeforums guided me away from the haas. Instead I picked up a mori seiki. WAY more accurate, better surface finishes through rigidity that dwarfs the tormachs.

Look at the spindle of the tormach compared to the spindle of a haas and then compare the spindle of the haas to a mori.

The tormach 440 is on the far end of hobbiest vs real machine. I know it sucks to hear but it is what it is. I'd grab a haas before the tormach for sure. You'll be limited on the tooling that weak motor can run as well as the rigidity it lacks.

I'm not sure I have the room or budget, but I'll look up Mori Seiki!

 

[shinyedges]

I'm not sure I have the room or budget, but I'll look up Mori Seiki!

A good used one can be had if you know where to look and will go get it.

 

[Contender Machine]

I would have to fully agree with shinyedges on trying to get a heavier built machine if you want to cut steel. Personally, I would buy an old, half worn out 40 taper mill long before I’d buy a little machine like a Tormach. There is absolutely no replacement for mass and rigidity when it comes to CNC machining. If you are handy with mechanical stuff you can likely fix any small problems that may arise with a used machine. Though I will say a lot of knives do get machined on tormachs. A used haas or doosan would be an excellent entry level mill. A mori seiki would be even better.

As for end mills I would recommend onlinecarbide.com. Ironically there website is kind of terrible and they look like some shady cheap made carbide company but there products are anything but. I’ve ran them hard (like 12000 rpm and 550 ipm in 4140 on a 1/2 and mill) against the likes of YG1 and Helical and the onlinecarbide end mills always out perform. If you call them they will make any tool you want.

There’s about 10,001 variables in CNC machining but starting with an assortment of 4 flute end mills up to 1/2 inch would be where I’d start. In a small machine like a tormach I think you’d probably be better off roughing with nothing bigger than a 3/8 anyway.

Edit: I’m not trying to discourage you and say a tormach will never work because they do but you will have less issues and better products with a heavier machine guaranteed.

 

[kuraki]

3D milling bevels is about the least efficient way to do it. Though for one offs it's probably the easiest way to set up. I 3D milled this from a solid block of S7 a few years ago on a 50 taper Haas.

 

[herromynameis]

I would have to fully agree with shinyedges on trying to get a heavier built machine if you want to cut steel. Personally, I would buy an old, half worn out 40 taper mill long before I’d buy a little machine like a Tormach. There is absolutely no replacement for mass and rigidity when it comes to CNC machining. If you are handy with mechanical stuff you can likely fix any small problems that may arise with a used machine. Though I will say a lot of knives do get machined on tormachs. A used haas or doosan would be an excellent entry level mill. A mori seiki would be even better.

As for end mills I would recommend onlinecarbide.com. Ironically there website is kind of terrible and they look like some shady cheap made carbide company but there products are anything but. I’ve ran them hard (like 12000 rpm and 550 ipm in 4140 on a 1/2 and mill) against the likes of YG1 and Helical and the onlinecarbide end mills always out perform. If you call them they will make any tool you want.

There’s about 10,001 variables in CNC machining but starting with an assortment of 4 flute end mills up to 1/2 inch would be where I’d start. In a small machine like a tormach I think you’d probably be better off roughing with nothing bigger than a 3/8 anyway.

Edit: I’m not trying to discourage you and say a tormach will never work because they do but you will have less issues and better products with a heavier machine guaranteed.

Not discouraged at all. I welcome your honest feedback! I hear you loud and clear. I know the 440 would need to be replaced, but for lack of space reasons at the moment, I may have to go Tormach for proof of concept first. I have no problem running slow and steady until I reach a point of larger demand.

Thank you for the onlinecarbide recommend! I'll definitely check them out. I'll grab an assortment of 4 flutes at .5 in max on your advice. Love having rules of thumb to go by. Thanks so much Contender.

 

[herromynameis]

3D milling bevels is about the least efficient way to do it. Though for one offs it's probably the easiest way to set up. I 3D milled this from a solid block of S7 a few years ago on a 50 taper Haas.

Very cool, thanks for sharing, kuraki! Yea, I've spent the last few years designing other things like buildings and installations in 3D for work, so when I picked this up I immediately started 3D modeling my prototypes first. Now I'm wanting to streamline that process from the model into an accurate physical manifestation as efficiently as possible, hence the determination to CNC.

 

[kuraki]

Looking at this a little deeper now that I'm not on my phone.

To put it bluntly, I think buying that Tormach to 3D mill bevels will be a complete and total waste of your time and money. For $20k you could get a relatively late model used Tormach 1100 with a BT spindle or an older HAAS VF1 or VF2 with a 40 taper.

That said, if you toss the idea of machining bevels and use the machine for profiling blades, making holes, 3D milling handles and aluminum tooling for forming kydex, I think it would work out well for you. Here's the thing about CNC most people don't conceptualize. If you do *everything* in the machine, you have ass time. Now you might say that's ok because it's leisure time or design time or programming time. But by doing that you're severely extending the ROI on buying the machine. Because of how significantly, incredibly, painfully slow that machine would be at milling bevels, by moving that single operation to a grinder, you could double, triple, maybe quadruple your output. For example:

Simple 3 piece full tang fixed blade and sheath. You have the blade, two handle halves and the kydex. So at least 4 setups - but more than likely more depending how much machining you're going to do to each component.

Blade: Assume your stock is ground to thickness. You need to 1- drill some tooling holes in your stock. This could be done in the machine or manually on a drill press, they're not critical, they're just to hold your work down onto a fixture plate. Then before you machine the profile, you need to make holes for the handle. These need to be precise in form and position both for handle indexing, and to use as locating holes for flipping the blade over if you intend to machine bevels. You make those holes, and maybe some additional ones for lightening the tang. Option stop in the program to bolt down through those holes, so that your yet to be machined profiled knife doesn't fly away when you hit the last little bit of profile stock. Now you machine the profile. Depending on the material, hardness, thickness, etc variables, that 440 can probably do all this in lets say 1 hour. Option stop again and you remove the skeleton of material from the machine before you start beveling. Depending on the surface finish you want off the machine this could take anywhere from 1 hour and require A LOT of post processing finish work, or 8 hours with minute stepovers and spring passes for a next to complete surface finish. Then you have to flip it over and do it again. The point here, is that in that 2 to 16 hours of machine time to make bevels, there's likely no way that blade doesn't require post processing - at minimum it requires a micro bevel edge, but more than likely the surface finish on the bevel is so incongruent with the surface finish of the flats, you end up hand sanding or grinding it to something more palatable.

Handle pieces follow a similar process, at a far reduced time. From profiling to 3D contouring, you can run your machine probably 5 times faster because the material is so much easier to cut. So lets say from start to finish that's 1 hour of machine time for a finished handle. Your post processing could be nothing, like Carothers handle scales, or very simple, like a quick sandblasting or buffing. Either way very little manual time.

Sheath is even faster if you've made an aluminum mold. You manually press the mold, drop it on a fixture plate and in a generous 10 minutes have something ready to be assembled or folded at the seam.

Here's the thing, it would take me less than a hour to grind those bevels manually from stock to finish for a belt finish blade. Maybe 2 hours total for belt finish and hand sand. You have a minimum 1 hour run time for profiling and holemaking, 1 hour run time for the handles and 10 minutes for your sheath. Now you're building a complete knife every 2 hours and 15 minutes versus trying to get your little machine to run lights out and STILL require hand finishing.

I didn't run any simulations in CAM and I have a relatively simple knife in mind, so some of my estimates may be off, and you might say "well I don't care about production runs" - yep I get all that. The grander point still stands. 3D milling bevels is incredibly inefficient, and that machine is likely too small to do them the way (iirc) Carothers does them, with angled vise jaws and side milling, so if that's truly what you can afford, then you should look really hard at adding a grinder to your tooling list and do bevels outside of your machine. Because I understand this: "...from the model into an accurate physical manifestation as efficiently as possible, hence the determination to CNC" concept 100%, but the bevels themselves have little if any relationship to the other features modeled. Design your sheaths the right way and it won't matter one bit if there's some variability from knife to knife in the bevel. The handle doesn't care if this one is a saber grind and that one is a full flat grind or the next one is hollow ground. So there's little need to stabilize that process with CNC when the cost is so high to do so.

The knife I posted is probably the most expensive (cost) knife I've ever made. And I couldn't give it away I think I got $250 for it.

 

[herromynameis]

Looking at this a little deeper now that I'm not on my phone.

To put it bluntly, I think buying that Tormach to 3D mill bevels will be a complete and total waste of your time and money. For $20k you could get a relatively late model used Tormach 1100 with a BT spindle or an older HAAS VF1 or VF2 with a 40 taper.

That said, if you toss the idea of machining bevels and use the machine for profiling blades, making holes, 3D milling handles and aluminum tooling for forming kydex, I think it would work out well for you. Here's the thing about CNC most people don't conceptualize. If you do *everything* in the machine, you have ass time. Now you might say that's ok because it's leisure time or design time or programming time. But by doing that you're severely extending the ROI on buying the machine. Because of how significantly, incredibly, painfully slow that machine would be at milling bevels, by moving that single operation to a grinder, you could double, triple, maybe quadruple your output. For example:

Simple 3 piece full tang fixed blade and sheath. You have the blade, two handle halves and the kydex. So at least 4 setups - but more than likely more depending how much machining you're going to do to each component.

Blade: Assume your stock is ground to thickness. You need to 1- drill some tooling holes in your stock. This could be done in the machine or manually on a drill press, they're not critical, they're just to hold your work down onto a fixture plate. Then before you machine the profile, you need to make holes for the handle. These need to be precise in form and position both for handle indexing, and to use as locating holes for flipping the blade over if you intend to machine bevels. You make those holes, and maybe some additional ones for lightening the tang. Option stop in the program to bolt down through those holes, so that your yet to be machined profiled knife doesn't fly away when you hit the last little bit of profile stock. Now you machine the profile. Depending on the material, hardness, thickness, etc variables, that 440 can probably do all this in lets say 1 hour. Option stop again and you remove the skeleton of material from the machine before you start beveling. Depending on the surface finish you want off the machine this could take anywhere from 1 hour and require A LOT of post processing finish work, or 8 hours with minute stepovers and spring passes for a next to complete surface finish. Then you have to flip it over and do it again. The point here, is that in that 2 to 16 hours of machine time to make bevels, there's likely no way that blade doesn't require post processing - at minimum it requires a micro bevel edge, but more than likely the surface finish on the bevel is so incongruent with the surface finish of the flats, you end up hand sanding or grinding it to something more palatable.

Handle pieces follow a similar process, at a far reduced time. From profiling to 3D contouring, you can run your machine probably 5 times faster because the material is so much easier to cut. So lets say from start to finish that's 1 hour of machine time for a finished handle. Your post processing could be nothing, like Carothers handle scales, or very simple, like a quick sandblasting or buffing. Either way very little manual time.

Sheath is even faster if you've made an aluminum mold. You manually press the mold, drop it on a fixture plate and in a generous 10 minutes have something ready to be assembled or folded at the seam.

Here's the thing, it would take me less than a hour to grind those bevels manually from stock to finish for a belt finish blade. Maybe 2 hours total for belt finish and hand sand. You have a minimum 1 hour run time for profiling and holemaking, 1 hour run time for the handles and 10 minutes for your sheath. Now you're building a complete knife every 2 hours and 15 minutes versus trying to get your little machine to run lights out and STILL require hand finishing.

I didn't run any simulations in CAM and I have a relatively simple knife in mind, so some of my estimates may be off, and you might say "well I don't care about production runs" - yep I get all that. The grander point still stands. 3D milling bevels is incredibly inefficient, and that machine is likely too small to do them the way (iirc) Carothers does them, with angled vise jaws and side milling, so if that's truly what you can afford, then you should look really hard at adding a grinder to your tooling list and do bevels outside of your machine. Because I understand this: "...from the model into an accurate physical manifestation as efficiently as possible, hence the determination to CNC" concept 100%, but the bevels themselves have little if any relationship to the other features modeled. Design your sheaths the right way and it won't matter one bit if there's some variability from knife to knife in the bevel. The handle doesn't care if this one is a saber grind and that one is a full flat grind or the next one is hollow ground. So there's little need to stabilize that process with CNC when the cost is so high to do so.

The knife I posted is probably the most expensive (cost) knife I've ever made. And I couldn't give it away I think I got $250 for it.

This is a really, really thoughtful point, kuraki. You've given me a lot to think about. Here was my line of thinking which I would love for you to be critical of.

1. To some, 20k doesn't break the bank and is worth it especially if it is going straight into making ROI back into the machine. For me 20k is too hefty a price right now, and I have a bigger learning curve ahead of me than someone who might just get the bigger machine and crank out success. To be frank, I know that if I'm successful in my designs I will have tanked 10k or so into a poor production machine. But, if I'm unsuccessful(and so many are) I may be tanking 20k into a production machine. If in the knifemaking world you're a proven Lionel Messi telling me to buy the $300 cleats, I might be the 2nd grade co-ed team bench player in the shoe section at TJ Maxx thinking I'll start here.

2. My space and "shop" are limited currently. I have a work/live loft setup with my girlfriend. I don't have the room for much more than a Tormach 440, and also have to keep things quiet enough not to piss off the neighbors(So at the moment I may not have a choice but to run slow speed/feed anyway).

3. I have a day job that pays the bills and I won't be able to stand at the grinder consistently. I'd like to start a process, walk away, then help it to the next. The ultimate goal for this is to automate it enough that my time is freed to do computer work which pays much more than knives, at least currently. I'd like to run a full time knife business one day, but only when I have proof of concept and demand, and have figured out said automation to free myself from the common money=time dilemma of a pure by-hand maker, of whom I have great respect for. My gf's business has good demand, but it is tied directly to her time and if she wants more money that means more hours of by-hand with no exceptions - so her income stays directly fixed to her physical labor. I know a smaller CNC machine won't be scalable, but I believe the CNC process is. I can always go bigger later when it proves more prudent.

Ok, I've attempted my arguments here, let me know what you think. You raise a lot of good points. I think for a while I could hybridize my work (grinding bevels on CNC profiled blades) to compensate for lack of knowledge and speed up the process if I need to crank some out. Walter Sorrells has a funny video where he CNCs throwing knives but then just bevels them by hand anyway.

 

[kuraki]

This is a really, really thoughtful point, kuraki. You've given me a lot to think about. Here was my line of thinking which I would love for you to be critical of.

1. To some, 20k doesn't break the bank and is worth it especially if it is going straight into making ROI back into the machine. For me 20k is too hefty a price right now, and I have a bigger learning curve ahead of me than someone who might just get the bigger machine and crank out success. To be frank, I know that if I'm successful in my designs I will have tanked 10k or so into a poor production machine. But, if I'm unsuccessful(and so many are) I may be tanking 20k into a production machine. If in the knifemaking world you're a proven Lionel Messi telling me to buy the $300 cleats, I might be the 2nd grade co-ed team bench player in the shoe section at TJ Maxx thinking I'll start here.

It's a lot for anyone. I only picked that price out of the hat because optioned out, the 440 gets close to that price and I wasn't sure what level of options you're looking at. Regardless your total spend even with a minimal option set is going to be over $10k before you're really making parts. Your reasoning is sound with one exception. A "real" machine worth 20k today has about depreciated as far as it ever will, sans being completely wrecked. A 440 will likely be worth half it's purchase price in a very short time.

Now frame this a little differently like "I want to spend a max $10k to invest in my learning how to CNC machine stuff in my garage" and the 440 looks a lot better. Those are now sunken costs, the ROI is the knowledge gained, prototypes fleshed out, and maybe gives you the confidence to get into financing a bigger machine.

2. My space and "shop" are limited currently. I have a work/live loft setup with my girlfriend. I don't have the room for much more than a Tormach 440, and also have to keep things quiet enough not to piss off the neighbors(So at the moment I may not have a choice but to run slow speed/feed anyway).

Understandable. Double check that small actually means quiet. Is it brushless? Or is it going to scream like a harbor freight bandsaw?

3. I have a day job that pays the bills and I won't be able to stand at the grinder consistently. I'd like to start a process, walk away, then help it to the next. The ultimate goal for this is to automate it enough that my time is freed to do computer work which pays much more than knives, at least currently. I'd like to run a full time knife business one day, but only when I have proof of concept and demand, and have figured out said automation to free myself from the common money=time dilemma of a pure by-hand maker, of whom I have great respect for. My gf's business has good demand, but it is tied directly to her time and if she wants more money that means more hours of by-hand with no exceptions - so her income stays directly fixed to her physical labor. I know a smaller CNC machine won't be scalable, but I believe the CNC process is. I can always go bigger later when it proves more prudent.

Yeah, I understand what you're saying here, I just don't think you're adequately weighing the costs of running lights out. I don't necessarily mean in dollars spent. I'm primarily talking about time invested. Again, frame this as an educational expense and it's a different value proposition. But if you can only devote a couple hours a day to this project and are under the impression that's the amount of time you'll have to invest regularly to get results while you sleep, you're mistaken. Now you're looking at extending those operations days and days and days before you're likely confident enough to hit go and walk away. Particularly if you're buying a machine with no tool changer.

Ok, I've attempted my arguments here, let me know what you think. You raise a lot of good points. I think for a while I could hybridize my work (grinding bevels on CNC profiled blades) to compensate for lack of knowledge and speed up the process if I need to crank some out. Walter Sorrells has a funny video where he CNCs throwing knives but then just bevels them by hand anyway.

I think if you say I want to invest $10k to learn CNC milling in my garage by prototyping knife parts, and recognize that at 1-2 hours per day it may take years to get to a point with your designs, knowledge and confidence that buying a more capable machine becomes less of a risk, then you have a good plan, and a machine that can still be useful even in the presence of a more capable machine. But anticipating it to make you any money by itself is I think folly. It's like being in a boat that's taking on water and baling with a spoon. You can't bail fast enough, long enough, to over come the leak. Even if it's "better than nothing" the boat is going to sink. But if you had a 5 gallon bucket you could perhaps keep it afloat indefinitely.

Some might say spending that $10k on tech school night classes will get you further and farther, but those come with their own constraints and limitations, particularly when you have a day job.

 

[TILLER]

I have a Tormach 1100. I enjoy making knives with it. Tormach has a lot of advantages to a hobbyist. You can get parts relatively cheap. I replaced a ball screw and a couple r8 tts collets. Collets were from crashes. You are going to crash it unless you are already an experienced machinist and programmer. You can buy a new spindle from tormach if you had to. Check spare parts on a Mori.

There is a good hobby level following for tormachs and fusion.

I would agree that if you are going to try to make knives for a living, you’d be far better off with a better machine. I’ve had times with more free time to put towards knifemaking where I wished I had bought a used Haas or something instead. Most of the time I’m happy with the tormach and the money I have in it. If you are making knives for fun in your spare time and will sell them here and there, it’s great.

A tool changer is also a big consideration. If you don’t have one you either sit there and change tools manually, which defeats the purpose of being able to work on other things, or find ways to use fewer tools. My latest fixture plate takes barstock to a knife and does the handles in one plate. No changing it out and rezeroing. I programmed as much as I could with a 1/8 stub end mill. The whole knife except engravings and chamfers is done with a 1/8 end mill. It would be a waste to do that with an industrial machine with a tool changer, but it allows me to have more time between tool changes and really doesn’t take much, if any, more time.

But back to the question of what tooling, I’d start with programming and then buying tools based on what you need. But 1/8, 3/16, 1/4 end mills, drills based on what you need, a chamfer mill and an engraving mill are my most used tools for blades. The handles get made with a 3/16 end mill for the holes, an 82 degree countersink, and a 1/4 or 3/8 ball mill for profiling and contouring.

You will need to be able to tap holes. Probably easiest to get going with manual taps. I also use thread mills with the single cutter. 1/4-20 is my go to for holes for the fixture.

I have been buying the uncoated 1/8 stub mills from carbidetoolsource because they are cheap in 5 packs. I use one per knife. Flood coolant. Makes it easy for figuring tool life.

I’ll add that my machining time for 1/8 end mill, 3/16 D2, 4.25” blade is just under 17 minutes per side; for the bevels. That’s faster than I could grind it. And more accurate. I follow up with 220 hand sanding and go from there.

 

[herromynameis]

It's a lot for anyone. I only picked that price out of the hat because optioned out, the 440 gets close to that price and I wasn't sure what level of options you're looking at. Regardless your total spend even with a minimal option set is going to be over $10k before you're really making parts. Your reasoning is sound with one exception. A "real" machine worth 20k today has about depreciated as far as it ever will, sans being completely wrecked. A 440 will likely be worth half it's purchase price in a very short time.

Now frame this a little differently like "I want to spend a max $10k to invest in my learning how to CNC machine stuff in my garage" and the 440 looks a lot better. Those are now sunken costs, the ROI is the knowledge gained, prototypes fleshed out, and maybe gives you the confidence to get into financing a bigger machine.



Understandable. Double check that small actually means quiet. Is it brushless? Or is it going to scream like a harbor freight bandsaw?



Yeah, I understand what you're saying here, I just don't think you're adequately weighing the costs of running lights out. I don't necessarily mean in dollars spent. I'm primarily talking about time invested. Again, frame this as an educational expense and it's a different value proposition. But if you can only devote a couple hours a day to this project and are under the impression that's the amount of time you'll have to invest regularly to get results while you sleep, you're mistaken. Now you're looking at extending those operations days and days and days before you're likely confident enough to hit go and walk away. Particularly if you're buying a machine with no tool changer.



I think if you say I want to invest $10k to learn CNC milling in my garage by prototyping knife parts, and recognize that at 1-2 hours per day it may take years to get to a point with your designs, knowledge and confidence that buying a more capable machine becomes less of a risk, then you have a good plan, and a machine that can still be useful even in the presence of a more capable machine. But anticipating it to make you any money by itself is I think folly. It's like being in a boat that's taking on water and baling with a spoon. You can't bail fast enough, long enough, to over come the leak. Even if it's "better than nothing" the boat is going to sink. But if you had a 5 gallon bucket you could perhaps keep it afloat indefinitely.

Some might say spending that $10k on tech school night classes will get you further and farther, but those come with their own constraints and limitations, particularly when you have a day job.

Love this, Kuraki. Thanks so much for such a well thought out response. You're really helping me be introspective on my mindset going into this. I can't help but be optimistic about making the 440 work for me in short time, so it's good to hear a reality check that I'll likely be stuck in problem-solving mode much much longer than I anticipate, let alone make a dollar off it. I'm definitely able to spend more time than 2 hours a day on the digital side of the project, messing around on fusion360 and tool paths and such from a desk but it'll probably be the time at the machine that I'll be short on. I'm not the hands-on type as much as the sit and think type, so I'm really wanting to index on that in this way. Again, you're really helping me stay grounded here.

 

[herromynameis]

I have a Tormach 1100. I enjoy making knives with it. Tormach has a lot of advantages to a hobbyist. You can get parts relatively cheap. I replaced a ball screw and a couple r8 tts collets. Collets were from crashes. You are going to crash it unless you are already an experienced machinist and programmer. You can buy a new spindle from tormach if you had to. Check spare parts on a Mori.

There is a good hobby level following for tormachs and fusion.

I would agree that if you are going to try to make knives for a living, you’d be far better off with a better machine. I’ve had times with more free time to put towards knifemaking where I wished I had bought a used Haas or something instead. Most of the time I’m happy with the tormach and the money I have in it. If you are making knives for fun in your spare time and will sell them here and there, it’s great.

A tool changer is also a big consideration. If you don’t have one you either sit there and change tools manually, which defeats the purpose of being able to work on other things, or find ways to use fewer tools. My latest fixture plate takes barstock to a knife and does the handles in one plate. No changing it out and rezeroing. I programmed as much as I could with a 1/8 stub end mill. The whole knife except engravings and chamfers is done with a 1/8 end mill. It would be a waste to do that with an industrial machine with a tool changer, but it allows me to have more time between tool changes and really doesn’t take much, if any, more time.

But back to the question of what tooling, I’d start with programming and then buying tools based on what you need. But 1/8, 3/16, 1/4 end mills, drills based on what you need, a chamfer mill and an engraving mill are my most used tools for blades. The handles get made with a 3/16 end mill for the holes, an 82 degree countersink, and a 1/4 or 3/8 ball mill for profiling and contouring.

You will need to be able to tap holes. Probably easiest to get going with manual taps. I also use thread mills with the single cutter. 1/4-20 is my go to for holes for the fixture.

I have been buying the uncoated 1/8 stub mills from carbidetoolsource because they are cheap in 5 packs. I use one per knife. Flood coolant. Makes it easy for figuring tool life.

I’ll add that my machining time for 1/8 end mill, 3/16 D2, 4.25” blade is just under 17 minutes per side; for the bevels. That’s faster than I could grind it. And more accurate. I follow up with 220 hand sanding and go from there.

TILLER, my man. It's funny you should comment, because yesterday I bookmarked your example you posted in the "3d machining a fixed blade" thread from 2020. I've been following Aaron Gough's work closely, and it indeed looks super finnicky and time consuming to dial in properly. On top of that, if I'm trying out multiple designs, the idea of retuning his fixturing process for every knife makes me want to jump headfirst into a shark tank.

I saved your example as my go-to because like you said, you're able to do so much work on one side via a single end mill if necessary, without changing the fixture. I loved the simple approach of beveling but maintaining the final edge thickness around the blade and eliminating the need for extra fixture and clamp features. This appears to me just as stable as Gough's methods. I'm curious how you're shaping the handles as well on the same fixture? Have you changed your method since that post from 2020? I'm a sponge here.

These tool tips are great. Taking serious notes. I saw you've mentioned before you used 1/4" lakeshore carbide but switched to 1/8 stubby uncoated. Find 1/8 better for some reason?

Aha, 17 mins is blazing fast (Although it sounds maybe at that speed it'll be louder than if I ran it a little more conservatively?). Do you think a Tormach is capable of working on hardened steel? I use 1095. You said you cnc bevel, then hand sand to completion, but where is hardening in your process? I've been hardening in a kiln and upon oil quench it seems it would need at least some grinding again from scaling etc.

If I can make my work look as good as yours does within a year, which is a tall order I'll be a very happy man.

 

[TILLER]

Disclaimer, I’m just a guy who likes to make knives, I have not made a living making them. I learned machining from the internet and YouTube for the most part, so my knowledge is narrow compared to a machinist. I think setups/fixturing is an interesting and critical part of cnc knifemaking. I’d be very interested to see what other people have come up with. I’ve tried several different methods of work holding and setups.

This is my current setup:

First op: Barstock is held by pitbull clamps. Downside of this is that they have a very short clamping range, so precision ground stock works great, but rough stock sometimes needs to be cleaned up to fit.
A 1/8 mill does almost everything, bores the holes, etc. That runs for a while, then engraving and chamfering. If I need to knock a few thou off the thickness I’ll put in a 1/4 end mill and face the stock here. If I need to take a bit off or take off that cpm scale/pitting I’ll do that here too, flipping it.
Second op: flip the barstock and screw it down. Again 1/8 end mill does everything but chamfers and engraving.
Handles op 1: same as the barstock, 3/16 end mill does holes, then an 82 degree countersink
Handles op 2: screwed down to the fixture as shown. Area is raised so a 1/4 ball mill can use the side flutes to profile, then the ball to contour the tops.

I use a 1/8 mostly because it can reach all the holes etc without being too large. I used to spot, drill, preream, and ream the holes. For putting scales on a blade, boring the holes and then finishing them to size with the same end mill works great. The threaded standoffs are up to .005 over sized anyway so no point in making .25 hole with multiple tool changes. The boring has been consistent.

I harden the blade after machining and finishing. So far I’ve only used air hardening steels. They stay very clean with foil wrap so cleanup after heat treat is re-hand sanding. Might be more efficient to harden a blank and then machine it and be done. That’s something I’d like to try sometime but haven’t. Some of the steels I like to use would be really hard to sand out machining marks by hand in a hardened state. I don’t see why a tormach couldn’t do hardened steel. I think you would have to nail speeds and feeds and it would be real slow.

For speeds and feeds I’ve found FSWizard pro to give working numbers on the first try almost every time when I set it to 70%. I was always having chatter with g wizard numbers.

I think the fixture could be improved by finding a way to clamp with more clamp range. I think I might make the next one bolt to the table instead of the vise.

A different setup would be needed for cranking out lots of knives from a big sheet of steel or handle material.

I’ve thought about trying oil hardening steel. I think I’d try doing one the same way but hardening with pbc powder and seeing if that gives enough protection. Could harden a blank but with this setup it would be a barstock blank, so I’d worry about getting good through hardening. A different setup where you have a profiled blank, then heat treat, then do the bevels might work.

Side note, I give a .01 or .015 step over for the blade flats and .001 for the plunge. It seems to be a good compromise between speed and finish. I’ve tried ball and bull end mills but they don’t seem to give any better of a finish, with the parallel tool path.